Extrude Fails

famadorian

I was on a roll, creating lots of lofts and then extruding them, then suddenly it wouldn't work on one and it just throws the normal non-intuitive "can't regenerate" message.

Is there any way to get more sensical error messages so that I can figure out what's wrong?;)



Here's the public document: 
https://cad.onshape.com/documents/70d70cf1b954c030847ece24/v/569d1fc66d020cf1308e7410/e/d8b4ad7ea70fdf1769c91ad4

jakeramsley

famadorian said:

MBartlett21 said:

@famadorian
The face may not be quite planar.
Pease try this FS, which supports non-planar faces:
https://cad.onshape.com/documents/24819ddab7dc83c810eb8246
You may have to specify a direction using two points or a directional face

The loft is between two straight curves, so the face must be planar? Also, why doesn't the error tell me it's not planar, if that's the problem?

Also, not sure what you mean with FS? I looked at your document, but it doesn't use a FS function?;)

If you look at the vertices (and their resultant unit vectors), the loft doesn't create a planar surface:

vertices:

v1 = [-835.72000, 6578.46498, -1243.00003]

v2 = [-835.72000, -2009.53507, -1243.00003]

v3 = [-835.72000, 6578.46498, -4668.00022]

v4 = [-835.70999, -2009.53507, -4668.00022]

line vectors:

l1 = (v2 - v1) =[0, 1, 0]

l2 = (v4 - v3) = [-1.16558×10^-6, 1, 0]

Going from l1 to l2 will require a twist, which makes the resulting surface not planar.

john_mcclary

That is weird.

But Thicken does work, and is probably more appropriate for what you are doing anyway

MBartlett21

@famadorian
The face may not be quite planar.
Pease try this FS, which supports non-planar faces:
https://cad.onshape.com/documents/24819ddab7dc83c810eb8246
You may have to specify a direction using two points or a directional face

famadorian

MBartlett21 said:

@famadorian
The face may not be quite planar.
Pease try this FS, which supports non-planar faces:
https://cad.onshape.com/documents/24819ddab7dc83c810eb8246
You may have to specify a direction using two points or a directional face

The loft is between two straight curves, so the face must be planar? Also, why doesn't the error tell me it's not planar, if that's the problem?

Also, not sure what you mean with FS? I looked at your document, but it doesn't use a FS function?;)

MBartlett21

@famadorian
It does not tell you it isn't planar. It just doesnt accept the selection.
The faces and sketch regions to extrude box in your extrude is empty.


My document has a FS feature that you can add to your toolbar called Extrude
It allows you to specify a direction and also do a thin-feature extrude

jakeramsley

famadorian said:

MBartlett21 said:

@famadorian
The face may not be quite planar.
Pease try this FS, which supports non-planar faces:
https://cad.onshape.com/documents/24819ddab7dc83c810eb8246
You may have to specify a direction using two points or a directional face

The loft is between two straight curves, so the face must be planar? Also, why doesn't the error tell me it's not planar, if that's the problem?

Also, not sure what you mean with FS? I looked at your document, but it doesn't use a FS function?;)

If you look at the vertices (and their resultant unit vectors), the loft doesn't create a planar surface:

vertices:

v1 = [-835.72000, 6578.46498, -1243.00003]

v2 = [-835.72000, -2009.53507, -1243.00003]

v3 = [-835.72000, 6578.46498, -4668.00022]

v4 = [-835.70999, -2009.53507, -4668.00022]

line vectors:

l1 = (v2 - v1) =[0, 1, 0]

l2 = (v4 - v3) = [-1.16558×10^-6, 1, 0]

Going from l1 to l2 will require a twist, which makes the resulting surface not planar.

john_mcclary

Really, all the lofts and extrudes are overkill

just extrude your surfaces, then thicken
https://cad.onshape.com/documents/d42e6f41dfe15f73214cc08f/w/9f4e16f982213c9119a76ed0/e/85c5608385533392b45428ce

Turn 50 features into 2

famadorian

john_mcclary said:

That is weird.

But Thicken does work, and is probably more appropriate for what you are doing anyway

Thicken it is;) Thank you

famadorian

MBartlett21 said:

@famadorian
It does not tell you it isn't planar. It just doesnt accept the selection.
The faces and sketch regions to extrude box in your extrude is empty.


My document has a FS feature that you can add to your toolbar called Extrude
It allows you to specify a direction and also do a thin-feature extrude

Ah, it's a FeatureScript called Extrude in there;) Got it; thanks.